Delamination modeling of composite plate using VCCT

[GauthamBP]

Hello there!

I am attempting to conduct a delamination study of a square composite plate with a hole using the VCCT technique. I chose the VCCT because I intend on doing a low cycle fatigue analysis of the model later on. I had attempted this technique on a double cantilever beam problem with success. My composite plate consists of 20 layers. The model has an elliptical initial delamination near the hole, and I am trying to model delam between the first and second layers.

I have split the model into 2 parts, the bottom portion containing 19 layers and the top portion containing a single layer. I have established contact between the 2 parts everywhere except for the elliptical region I want the initial delam to be in. When I run a static simulation I find that the model keeps rotating, which shoudn't be the case. Could anyone suggest a reason as to why the model keeps rotating? I have applied surface tractions as loads.

I have attached the input file below. I have resricted motion in the z direction at all the side surfaces, and restricted motion at one corner in the x, y and z direction. The model appears to rotate around this fixed corner. The loads applied are equal in magnitude and have a zero resultant moment about this fixed corner. Please do help!

 

[FEA way]

Could you also share a picture of your model showing boundary conditions ? It looks like they are insufficient to constrain the 3D solid model against all 6 rigid body motions.

 

[GauthamBP]

Hello FEA way,

I have attached a pic depicting the boundary conditions. I should mention that the total thickness of the model is 3mm, the top portion containing a single layer is 0.15mm thick while the bottom portion containing 19 layers is 2.85 mm thick.

 

[FEA way]

Yes, apparently the model is underconstrained. You eliminated Z translation but it can still rotate about this node. Imagine that this is a planar model. Constraining one node in all directions is not enough, you need more nodes to prevent rotations (2 will be enough). Modal analysis is the best way to find out which rigid body motions are still unconstrained (they can be observed at frequencies close to zero).

 

[GauthamBP]

Hello FEA Way,

Could you guide me as to how to do this modal analysis and what nodes to constrain rotations for? I should also mention that when I applied the same boundary conditions for a shell model without any bonding i.e, just a shell with 20 layers of composite, the model didn't rotate. I had concluded that there was some problem caused due to the VCCT bonding as a result. Am I looking at it the wrong way?

 

[FEA way]

You can use 3-2-1 method to constrain your model. In this method you fix translations at 3 nodes, first one in all 3 directions, second one in 2 directions and last one in 1 direction. You can find the description of this method in some articles, there you will see which nodes to constrain.

To perform modal analysis replace static general step with frequency step, set the number of eigenfrequencies for extraction (6 are enough) and that's it (apart from supressing features that are not necessary for this simulation).